UpdatedLagrangianStressDivergence

Enforce equilibrium with an updated Lagrangian formulation in Cartesian coordinates.

Description

The UpdatedLagrangianStressDivergence kernel calculates the stress equilibrium residual in the current configuration using the cauchy_stress (the Cauchy stress). This kernel provides the residual for Cartesian coordinates and the user needs to add one kernel for each dimension of the problem. Alternatively, the TensorMechanics/MasterAction simplifies the process of adding the required kernels and setting up the input parameters.

Residual, Jacobian, and stabilization

For large deformation kinematics the kernel applies the residual $var element = document.getElementById("moose-equation-f906472a-96e6-4b2f-8608-43969d056c0f");katex.render(" R^{\\alpha}=\\int_{v}\\sigma_{ik}\\phi_{i,k}^{\\alpha}dv", element, {displayMode:true,throwOnError:false});$ with the corresponding Jacobian $var element = document.getElementById("moose-equation-3025d890-51d4-4ec9-b308-09264dcb4e0f");katex.render(" J^{\\alpha\\beta}=\\int_{v}\\left\\{ T_{ijkl}\\phi_{i,j}^{\\alpha}f_{km}g_{ml}^{\\beta}+\\sigma_{ij}\\left(\\phi_{k,k}^{\\alpha}\\psi_{ij}^{\\beta}-\\phi_{k,j}^{\\alpha}\\psi_{ik}^{\\beta}\\right)\\right\\} dv", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-f3bc1352-539d-4d44-adb4-24dd4204dc85");katex.render("\\sigma_{ik}", element, {displayMode:false,throwOnError:false});$ is the Cauchy stress, $var element = document.getElementById("moose-equation-8376a2e3-c1fb-4d63-8bf9-6a78c97eeb3e");katex.render(" T_{ijkl} = \\frac{\\partial \\sigma_{ij}}{\\partial \\Delta l_{kl}}", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-c8759ca4-954b-440d-82f9-05b75bf0032d");katex.render(" \\Delta l_{kl} = \\Delta F_{kM} F^{-1}_{Ml}", element, {displayMode:true,throwOnError:false});$ the incremental spatial velocity gradient, $var element = document.getElementById("moose-equation-d8a4b328-8f89-4b9c-baaa-55746c909616");katex.render("\\phi_{i,j}^{\\alpha}", element, {displayMode:false,throwOnError:false});$ are the test function gradients (with respect to the current coordinates) and $var element = document.getElementById("moose-equation-0bb48fae-1d82-48a0-b05d-e451f9e00460");katex.render(" g_{ij}^{\\beta} = \\frac{dF_{iK}}{d\\Upsilon^{\\beta}} F_{Kj}^{-1}", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-05d7a7ff-018a-4a25-966d-496600a22feb");katex.render("\\Upsilon^\\beta", element, {displayMode:false,throwOnError:false});$ the discrete (nodal) displacements. For the unstabilized case $var element = document.getElementById("moose-equation-4c39cbc5-c4a2-4266-92ab-bd8c3c02dd35");katex.render(" g_{ij}^{\\beta} = \\psi_{i,j}^{\\beta}", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-d58b951e-9544-4f52-a6af-856f429885d9");katex.render("\\psi_{i,j}^{\\beta}", element, {displayMode:false,throwOnError:false});$ the trial function gradients with respect to the current coordinates.

The residual and Jacobian degenerate to $var element = document.getElementById("moose-equation-e8d945ac-eda1-474a-8902-cd3a97aa2860");katex.render(" R^{\\alpha}=\\int_{v}s_{ij}\\phi_{i,j}^{\\alpha}dv", element, {displayMode:true,throwOnError:false});$ and $var element = document.getElementById("moose-equation-8cd7a01c-82c4-46b0-8673-1d99ace215a0");katex.render(" J^{\\alpha\\beta}=\\int_{V}\\phi_{i,j}^{\\alpha}C_{ijkl}g_{kl}^{\\beta}dV", element, {displayMode:true,throwOnError:false});$ for the small deformation case, with $var element = document.getElementById("moose-equation-37cec52a-be5e-4d00-b02e-3baed286d760");katex.render("s_{ij}", element, {displayMode:false,throwOnError:false});$ the small stress, $var element = document.getElementById("moose-equation-5a36702e-b094-4b3e-b538-9dfaabd97503");katex.render(" C_{ijkl} = \\frac{\\partial s_{ij}}{\\partial \\varepsilon_{kl}}", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-f34bc834-b6c3-4b54-994e-c06a07c47493");katex.render("\\varepsilon_{kl}", element, {displayMode:false,throwOnError:false});$ the small strain and $var element = document.getElementById("moose-equation-45c2426b-24f3-4702-a9f2-dcb435c624e6");katex.render(" g_{kl}^{\\beta} = \\psi_{k,l}^{\\beta}", element, {displayMode:true,throwOnError:false});$ for the unstabilized case. The large_kinematics flag controls the kinematic theory. For this kernel use_displaced_mesh must be set to true if large_kinematics is true so that the volume integrals and gradients are with respect to the current coordinates.

For the Jacobian the small deformation $var element = document.getElementById("moose-equation-93bfaef3-4a73-46ed-b1ef-597063a8e824");katex.render(" \\phi_{i,j}^{\\alpha}C_{ijkl}g_{kl}^{\\beta}", element, {displayMode:true,throwOnError:false});$ term and the large deformation term $var element = document.getElementById("moose-equation-8a5b33d5-d5b6-48b8-bf3f-f07e55321d43");katex.render(" T_{ijkl}\\phi_{i,j}^{\\alpha}f_{km}g_{ml}^{\\beta}", element, {displayMode:true,throwOnError:false});$ are identical (assuming the incremental deformation gradient is the identity and the deformation gradient degenerates to the small strain for the small deformation case) and involve the constitutive model. These are then called the "material" part of the Jacobian. The remaining large deformation term $var element = document.getElementById("moose-equation-1451318e-dfd7-453a-bea1-c96d19a0ac87");katex.render(" \\sigma_{ij}\\left(\\phi_{k,k}^{\\alpha}\\psi_{ij}^{\\beta}-\\phi_{k,j}^{\\alpha}\\psi_{ik}^{\\beta}\\right)", element, {displayMode:true,throwOnError:false});$ involves the current stress and the updated geometry and so it is called the "geometric" part of the Jacobian.

The constitutive model needs to provide the Cauchy stress and the derivative of that stress with respect to the increment in the spatial velocity gradient. However, the material system provides a common interface to define the constitutive model with any stress and strain measures that are convient, translating the user-defined stress and Jacobian to the correct form automatically. Note that if the model is rotationally invariant then $var element = document.getElementById("moose-equation-ec096097-ee2d-4dba-8ed2-57ecaec5fa17");katex.render(" \\Delta l_{kl} = \\Delta d_{kl}", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-a3e71625-c9c5-4c5a-8d92-7a41f6446789");katex.render("\\Delta d_{kl}", element, {displayMode:false,throwOnError:false});$ is the increment in the material deformation rate, equal to the increment in the logarthmic strain Freed (2014).

The kernel is compatible with the $var element = document.getElementById("moose-equation-f43e5809-9439-45f2-bc27-e1dff247cbc6");katex.render("\\bar{\\boldsymbol{F}}", element, {displayMode:false,throwOnError:false});$ modification of the strains to stabilize the problem for incompressible or nearly incompressible deformation. This form of stabilization does not modify the residual equation, though the modified strain does change the constitutive model stress update. The strain modification does affect the Jacobian by altering the definition of the gradient tensors. With the modified strains applied these become for small deformations $var element = document.getElementById("moose-equation-206df677-1a7c-4298-985c-04d50e974b25");katex.render(" g_{ij}^{\\beta}=\\psi_{i,j}^{\\beta}-\\frac{1}{3}\\left(\\psi_{kk}^{\\beta}-\\bar{\\psi}_{kk}^{\\beta}\\right)\\delta_{ij}", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-c627a6bb-7f11-4ac8-974e-ac028f428309");katex.render(" \\bar{\\psi}_{i,j}^{\\beta}=\\frac{1}{v}\\int_{v}\\psi_{i,j}^{\\beta}dv", element, {displayMode:true,throwOnError:false});$ and for large deformations $var element = document.getElementById("moose-equation-6c68a24d-70fd-4185-aa56-fe5052b2d70a");katex.render(" g_{iJ}^{\\beta}=\\left[\\psi_{i,j}^{\\beta}-\\frac{1}{3}\\delta_{ij}\\left(\\psi_{k,k}^{\\beta}-\\bar{\\psi}_{k,k}^{\\beta}\\right)\\right]", element, {displayMode:true,throwOnError:false});$ with $var element = document.getElementById("moose-equation-2fa8388e-a135-48fa-8736-f61810cb21be");katex.render(" \\bar{\\psi}_{i,j}^{\\beta}=\\frac{1}{V}\\int_{V}\\psi_{i,K}^{\\beta}dV\\bar{F}_{Kj}^{-1}", element, {displayMode:true,throwOnError:false});$ and $var element = document.getElementById("moose-equation-7d59ea64-0691-4910-9611-dd4514049562");katex.render("\\bar{F}", element, {displayMode:false,throwOnError:false});$ the average deformation gradient, defined in the stabilization system documentation. Note this is a somewhat unusual integral for an updated Lagrangian model, but it follows to keep the derivative term consistent with the $var element = document.getElementById("moose-equation-6de50f17-9416-461c-b1e7-ab978771b462");katex.render("\\bar{\\boldsymbol{F}}", element, {displayMode:false,throwOnError:false});$ modification to the strains. The stabilize_strain flag controls if the kernel modifies the Jacobian to account for the stabilized strains.

`use_displaced_mesh`

The UpdatedLagrangianStressDiverence kernel is the only object in the new, Lagrangian Tensor Mechanics system that requires use_displaced_mesh to be set. The use_displaced_mesh flag should be set to true if and only if large_kinematics is also true. The kernel enforces this condition with an error.

Example Input File Syntax

The following illustrates manually including 3D stress equilibrium with the total Lagrangian formulation, using large deformation kinematics.

[Kernels]
  [sdx]
    type = UpdatedLagrangianStressDivergence
    variable = disp_x
    displacements = 'disp_x disp_y disp_z'
    component = 0
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdy]
    type = UpdatedLagrangianStressDivergence
    variable = disp_y
    displacements = 'disp_x disp_y disp_z'
    component = 1
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdz]
    type = UpdatedLagrangianStressDivergence
    variable = disp_z
    displacements = 'disp_x disp_y disp_z'
    component = 2
    use_displaced_mesh = true
    large_kinematics = true
  []
[]

Input Parameters

componentWhich direction this kernel acts in
C++ Type:unsigned int
Controllable:No
Description:Which direction this kernel acts in
displacementsThe displacement components
C++ Type:std::vector<VariableName>
Controllable:No
Description:The displacement components
variableThe name of the variable that this residual object operates on
C++ Type:NonlinearVariableName
Controllable:No
Description:The name of the variable that this residual object operates on

Required Parameters

base_nameMaterial property base name
C++ Type:std::string
Controllable:No
Description:Material property base name
blockThe list of blocks (ids or names) that this object will be applied
C++ Type:std::vector<SubdomainName>
Controllable:No
Description:The list of blocks (ids or names) that this object will be applied
eigenstrain_namesList of eigenstrains used in the strain calculation. Used for computing their derivatives for off-diagonal Jacobian terms.
C++ Type:std::vector<MaterialPropertyName>
Controllable:No
Description:List of eigenstrains used in the strain calculation. Used for computing their derivatives for off-diagonal Jacobian terms.
large_kinematicsFalseUse large displacement kinematics
Default:False
C++ Type:bool
Controllable:No
Description:Use large displacement kinematics
out_of_plane_strainThe out-of-plane strain variable for weak plane stress formulation.
C++ Type:std::vector<VariableName>
Controllable:No
Description:The out-of-plane strain variable for weak plane stress formulation.
prop_getter_suffixAn optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
C++ Type:MaterialPropertyName
Controllable:No
Description:An optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
stabilize_strainFalseAverage the volumetric strains
Default:False
C++ Type:bool
Controllable:No
Description:Average the volumetric strains
temperatureThe name of the temperature variable used in the ComputeThermalExpansionEigenstrain. (Not required for simulations without temperature coupling.)
C++ Type:std::vector<VariableName>
Controllable:No
Description:The name of the temperature variable used in the ComputeThermalExpansionEigenstrain. (Not required for simulations without temperature coupling.)

Optional Parameters

absolute_value_vector_tagsThe tags for the vectors this residual object should fill with the absolute value of the residual contribution
C++ Type:std::vector<TagName>
Controllable:No
Description:The tags for the vectors this residual object should fill with the absolute value of the residual contribution
extra_matrix_tagsThe extra tags for the matrices this Kernel should fill
C++ Type:std::vector<TagName>
Controllable:No
Description:The extra tags for the matrices this Kernel should fill
extra_vector_tagsThe extra tags for the vectors this Kernel should fill
C++ Type:std::vector<TagName>
Controllable:No
Description:The extra tags for the vectors this Kernel should fill
matrix_tagssystemThe tag for the matrices this Kernel should fill
Default:system
C++ Type:MultiMooseEnum
Options:nontime, system
Controllable:No
Description:The tag for the matrices this Kernel should fill
vector_tagsnontimeThe tag for the vectors this Kernel should fill
Default:nontime
C++ Type:MultiMooseEnum
Options:nontime, time
Controllable:No
Description:The tag for the vectors this Kernel should fill

Tagging Parameters

control_tagsAdds user-defined labels for accessing object parameters via control logic.
C++ Type:std::vector<std::string>
Controllable:No
Description:Adds user-defined labels for accessing object parameters via control logic.
diag_save_inThe name of auxiliary variables to save this Kernel's diagonal Jacobian contributions to. Everything about that variable must match everything about this variable (the type, what blocks it's on, etc.)
C++ Type:std::vector<AuxVariableName>
Controllable:No
Description:The name of auxiliary variables to save this Kernel's diagonal Jacobian contributions to. Everything about that variable must match everything about this variable (the type, what blocks it's on, etc.)
enableTrueSet the enabled status of the MooseObject.
Default:True
C++ Type:bool
Controllable:Yes
Description:Set the enabled status of the MooseObject.
implicitTrueDetermines whether this object is calculated using an implicit or explicit form
Default:True
C++ Type:bool
Controllable:No
Description:Determines whether this object is calculated using an implicit or explicit form
save_inThe name of auxiliary variables to save this Kernel's residual contributions to. Everything about that variable must match everything about this variable (the type, what blocks it's on, etc.)
C++ Type:std::vector<AuxVariableName>
Controllable:No
Description:The name of auxiliary variables to save this Kernel's residual contributions to. Everything about that variable must match everything about this variable (the type, what blocks it's on, etc.)
seed0The seed for the master random number generator
Default:0
C++ Type:unsigned int
Controllable:No
Description:The seed for the master random number generator
use_displaced_meshFalseWhether or not this object should use the displaced mesh for computation. Note that in the case this is true but no displacements are provided in the Mesh block the undisplaced mesh will still be used.
Default:False
C++ Type:bool
Controllable:No
Description:Whether or not this object should use the displaced mesh for computation. Note that in the case this is true but no displacements are provided in the Mesh block the undisplaced mesh will still be used.

Advanced Parameters

References

AD Freed. Hencky strain and logarithmic rates in lagrangian analysis. International Journal of Engineering Science, 81:135–145, 2014.

@article{freed2014,
    author = "Freed, AD",
    title = "Hencky strain and logarithmic rates in Lagrangian analysis",
    journal = "International Journal of Engineering Science",
    volume = "81",
    pages = "135--145",
    year = "2014",
    publisher = "Elsevier"
}

(moose/modules/tensor_mechanics/test/tests/lagrangian/cartesian/updated/patch/large_patch.i)

[Mesh]
  [base]
    type = FileMeshGenerator
    file = 'patch.xda'
  []
  [sets]
    input = base
    type = SideSetsFromPointsGenerator
    new_boundary = 'left right bottom top back front'
    points = '    0 0.5 0.5
                  1 0.5 0.5
                  0.5 0.0 0.5
               '
             '   0.5 1.0 0.5
                  0.5 0.5 0.0
                  0.5 0.5 1.0'
  []
[]

[GlobalParams]
  displacements = 'disp_x disp_y disp_z'
[]

[Variables]
  [disp_x]
  []
  [disp_y]
  []
  [disp_z]
  []
[]

[Kernels]
  [sdx]
    type = UpdatedLagrangianStressDivergence
    variable = disp_x
    displacements = 'disp_x disp_y disp_z'
    component = 0
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdy]
    type = UpdatedLagrangianStressDivergence
    variable = disp_y
    displacements = 'disp_x disp_y disp_z'
    component = 1
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdz]
    type = UpdatedLagrangianStressDivergence
    variable = disp_z
    displacements = 'disp_x disp_y disp_z'
    component = 2
    use_displaced_mesh = true
    large_kinematics = true
  []
[]

[AuxVariables]
  [strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_zz]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xz]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_yz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_zz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_yz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xz]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[AuxKernels]
  [stress_xx]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xx
    index_i = 0
    index_j = 0
    execute_on = timestep_end
  []
  [stress_yy]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_yy
    index_i = 1
    index_j = 1
    execute_on = timestep_end
  []
  [stress_zz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_zz
    index_i = 2
    index_j = 2
    execute_on = timestep_end
  []
  [stress_xy]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xy
    index_i = 0
    index_j = 1
    execute_on = timestep_end
  []
  [stress_xz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xz
    index_i = 0
    index_j = 2
    execute_on = timestep_end
  []
  [stress_yz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_yz
    index_i = 1
    index_j = 2
    execute_on = timestep_end
  []

  [strain_xx]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xx
    index_i = 0
    index_j = 0
    execute_on = timestep_end
  []
  [strain_yy]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_yy
    index_i = 1
    index_j = 1
    execute_on = timestep_end
  []
  [strain_zz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_zz
    index_i = 2
    index_j = 2
    execute_on = timestep_end
  []
  [strain_xy]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xy
    index_i = 0
    index_j = 1
    execute_on = timestep_end
  []
  [strain_xz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xz
    index_i = 0
    index_j = 2
    execute_on = timestep_end
  []
  [strain_yz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_yz
    index_i = 1
    index_j = 2
    execute_on = timestep_end
  []
[]

[BCs]
  [left]
    type = DirichletBC
    preset = true
    variable = disp_x
    boundary = left
    value = 0.0
  []

  [bottom]
    type = DirichletBC
    preset = true
    variable = disp_y
    boundary = bottom
    value = 0.0
  []

  [back]
    type = DirichletBC
    preset = true
    variable = disp_z
    boundary = back
    value = 0.0
  []

  [front]
    type = DirichletBC
    preset = true
    variable = disp_z
    boundary = front
    value = 0.1
  []
[]

[Materials]
  [elastic_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 1000.0
    poissons_ratio = 0.25
  []
  [compute_stress]
    type = ComputeLagrangianLinearElasticStress
    large_kinematics = true
  []
  [compute_strain]
    type = ComputeLagrangianStrain
    displacements = 'disp_x disp_y disp_z'
    large_kinematics = true
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Executioner]
  type = Transient
  dt = 1

  solve_type = 'newton'

  petsc_options_iname = -pc_type
  petsc_options_value = lu

  nl_abs_tol = 1e-10
  nl_rel_tol = 1e-10

  end_time = 1
  dtmin = 1.0
[]

[Outputs]
  exodus = true
[]